How to apply Rigid Body Element 2 (RBE2) in Ansys Mechanical?
Hello there. I have already read a past thread where Mr. Peter said that RBE2 and RBE3 refers to Rigid and Deformable behavior respectively of the remote point, when scoped to a geometry. From my understanding, RBE2 distributes the applied remote force equally to every face (no matter the distance between application of force and scoped faces) it is scoped to while adding huge stiffness to it so that it becomes rigid and doesn't deform, while RBE3 relaxes the stiffness and allows it deform (and the distribution of force depends on the distance from application of force). However, in ANSYS Mechanical, when I am trying to add Rigid behavior to a remote point, it is not distributing the remote force equally on every face even though the face is rigid (I mean to say is that under rigid behavior, the distibution of force is still dependable on the distance from application of remote force to any of the scoped faces).
And also, I want to confirm that does RBE2 still distributes the force equally to each face even if they have different surface areas?
Best Answers

peteroznewman Member
Both ANSYS and NASTRAN have what are called Rigid Elements. NASTRAN calls it RBE2, while ANSYS calls it CERIG. There is a Master or Independent node and there are Slave or Dependent nodes. Both RBE2 and CERIG do the same thing: enforce displacement equations between nodes. The effect is to create a rigid region. Forces are irrelevant to the solver, it is displacement equations that must be satisfied in the solution.
There can be a distance effect. If the Master/Independent node is located at the origin and is rotated by a small angle about the Z axis, then a Slave/Dependent node at X = 2 will move in the Y direction twice as far as a Slave/Dependent node at X = 1. But if the Master/Independent node is translated by a small distance along the Y axis, then both Dependent nodes at X = 1 and X = 2 will move by the same amount in the Y direction.
A Force load in ANSYS will distribute a force to all faces in proportion to their projected area. Is that what you mean by "equally"? If the faces are all coplanar, and the force is normal to the face, then the projected area is just the area of the face. If one face has 3x the area of a second face, the total area of the two faces is 4 and the larger face will have 3/4 of the force while the smaller face will have 1/4 of the force. The net force will pass through the centroid of the two areas. If you want the net force to pass through a specific point and not the centroid of the area, then you can use a Remote Force and ANSYS will allocate forces to the nodes in such a way that the net force passes through the chosen point.

peteroznewman Member
ANSYS creates a mathematical model, based on your inputs, and the solver finds equilibrium to a high degree of precision. That means all the forces computed precisely balance the applied force.
Accuracy has to do with how closely the mathematical model represents the physical reality. You are idealizing the physical reality by replacing a physical object with an idealized representation. You are taking away a physical object that distributes the force among three tube and replacing it with a perfectly rigid mathematical object. Hopefully, that is a good representation, but that is up to you. An alternative is to represent that object in the model and allow its flexibility to be included in the calculations.

peteroznewman Member
a fixed support on a face of a solid body, that face will not see any deformation i.e. no motion of the nodes, but still it will experience a stresses because of the nodes on that face have stress (coming from the integration points)
a fixed support on a face of a solid body, that face will not see any deformation i.e. no motion of the nodes, but
stillitthe elements will experienceastresses becauseofthe nodes onthatthe opposite face havestressdeformations (coming fromcreating stress at the integration points).So If the applied force is not passing through the centroid of the scoped faces, what I understood is that the applied force is shifted to the centroid of the scoped faces, and all of the faces will have now equal distribution of force (assuming the faces are of same area).
No, the faces will not have an equal distribution of force, even if they have the same area. A special case when equal distribution of force could happen is when the rigid remote force origin passes through the centroid of the three areas and the direction is parallel to the tube axis. This setup is what you might call a zero moment configuration.
When the force moves away from the centroid of the three faces (or tilts), the forces reduce on one side and increase in the opposite side. Yes, you could replace the offset force with a force and moment at the centroid. The solver just does its thing to solve for the static equilibrium.
A moment applied to a face of a solid body is always resolved to nodal forces over the area of the face of that solid body. Only Beam and Shell Elements can have a moment input to a vertex or an edge that is directly applied to nodes as a moment.
Answers
Rigid Behavior (like a Nastran RBE2) does not distribute force equally to each face.
Rigid Behavior does have infinite stiffness. The dependent nodes on the scoped surface can only move rigidly with the motion of the remote point (independent node).
Do you mean to say that the distribution of force on the scoped faces (and its nodes) still depends on the distance between the location of remote point (or remote force) as like in deformable behavior? If yes, then it means that the only difference between RBE2 and RBE3 is the deformability of the the scoped faces, thats it.
And also, as like in RBE3 where forces distribution is also dependable on the surface areas of the scoped faces, is it also true for RBE2 (rigid behavior)?
And if I want to distribute the force equally to each face (as like in NASTRAN RBE2), how can I do it in ANSYS Mechanical?
Both ANSYS and NASTRAN have what are called Rigid Elements. NASTRAN calls it RBE2, while ANSYS calls it CERIG. There is a Master or Independent node and there are Slave or Dependent nodes. Both RBE2 and CERIG do the same thing: enforce displacement equations between nodes. The effect is to create a rigid region. Forces are irrelevant to the solver, it is displacement equations that must be satisfied in the solution.
There can be a distance effect. If the Master/Independent node is located at the origin and is rotated by a small angle about the Z axis, then a Slave/Dependent node at X = 2 will move in the Y direction twice as far as a Slave/Dependent node at X = 1. But if the Master/Independent node is translated by a small distance along the Y axis, then both Dependent nodes at X = 1 and X = 2 will move by the same amount in the Y direction.
A Force load in ANSYS will distribute a force to all faces in proportion to their projected area. Is that what you mean by "equally"? If the faces are all coplanar, and the force is normal to the face, then the projected area is just the area of the face. If one face has 3x the area of a second face, the total area of the two faces is 4 and the larger face will have 3/4 of the force while the smaller face will have 1/4 of the force. The net force will pass through the centroid of the two areas. If you want the net force to pass through a specific point and not the centroid of the area, then you can use a Remote Force and ANSYS will allocate forces to the nodes in such a way that the net force passes through the chosen point.
I want to do this, have a rigid (nondeformable) faces scoped to a remote force, I know the location of remote force, but I want that force to be equally distributed to each face. For example, if the net total remote force is 100 N; then no matter if one face has a bigger surface area than other, or is closer to the remote force location than other, I want the force to get equally distributed (i.e. 50 N each) by keeping both the faces as rigid.
And can you kindly educate me with how does artificially stiffening a scoped face to a remote force (by using rigid behavior) affect my solution at that face and the overall body it is a part of?
Thank you.
Here is a 2D illustration of the deformation of a flat circular surface, clamped on the edge, with a center face where a Remote Force is applied. The difference between using Rigid and Deformable behavior is clear.
If you want more specific guidance for your model, please reply with some images showing the overall geometry, the faces you want to be rigid, the direction of the force and the location where you want the net force to pass through. What is fastened to these faces to make them rigid?
Sir, first of all, thank you for your helpful answers.
But I want to clear somethings. For example, I have a structure which will be manufactured later and the expected loading condition is known. However, I am more concerned and thoughtful of the solution and results that I will get from ANSYS Static Structural. By the algorithm used by ANSYS solver, I will see some stress and displacement results within the whole structure. And that will depend on how much portion of that total remote force is taken by each of the scoped faces of the geometry (rather it be rigid or deformable).
Now assuming I know that the scoped faces will behave rigid in reality as well when that remote force is applied to them in reality, but how can I be sure that in reality those faces will take exactly the same amount or portion of that total remote force as calculated ANSYS. First I was confused about the RBE2 and RBE3 and its relation in ANSYS to rigidity and deformability of the scoped surfaces, but now my focal point is to know if ANSYS will correctly compute the portion of remote forces that will be expected in reality as well (assuming that the surface area of all the scoped faces is different from each other).
I was asking to distribute the remote force equally on each of the scoped rigid surface because I thought they will be distributed equally in reality as well.
The closer the model is to reality, the more likely the model captures what happens in reality.
Remote Forces are best used when a load is applied at a known point in space. For example, there is a bolt hole where an eye bolt will be inserted and a 500 kg mass will be supported. If this bolt hole is at the end of a 4 m long cantilevered structure bolted to the wall, you already know that the high stress is going to be near the wall. You also know that the stress will gradually reduce from the wall out to the bolt hole. It is a fine idea to cut away the outer 2 m of the cantilever structure and just keep the 2 m section that attaches to the wall. A remote force is created at a point 4 m from the wall, and scoped with rigid behavior to the cut faces/edges of the structure 2 m away from the wall. The high stress point is somewhere in the structure between 0 and 1 m from the wall, a long way from the cut boundary, and the stress is identical to the stress from a full model, but it solves faster because half the model was replaced by the remote force.
Please describe the physical load, show where the load is applied and what parts the load travels through to get to the Fixed Support. Insert images into your reply.
Okay I will try to explain using this model.
The remote force attached to the scoped geometries is of rigid behavior. Although the surface areas of all the scoped surfaces is same right now, but the problem is; depending upon the location of this remote point, the reaction forces in each of the three of above solid tubes will change. I have already tried that with a different location of remote point. I am trying to make the circular tubes as light weight as possible, therefore reach a safety factor of close to 1. The tubes are made of material Steel. Now I need to be confident that the portion of the remote force taken by each tube is exactly or closest to that experienced by the them in reality under the same condition, otherwise if not, there might be a failure in reality in any or all of them. I don't know the algorithm behind the calculation of distribution of remote force to its scoped faces, if I can know that somehow that would be very much beneficial for me.
And one more thing, I am baffled to see stresses on the rigid faces (which donot deform), rather it be fixed support or the rigid behavior faces where remote force is scoped to.
To answer your last question, it is normal to see stresses on elements next to fixed or rigidly supported faces. Consider a cantilever beam, the highest stress is at the fixed end. The element has some thickness and there are 8 nodes on a linear hex element. While four nodes on the fixed side didn't move, the four nodes on the other side of the element moved a lot. The stress is not computed at the nodes, but rather at points on the inside of the element. From the element's point of view, it sees a large relative displacement between the 8 nodes and computes a stress from that, and extrapolates that stress out to the nodes.
You are describing an optimization problem: Minimumize the weight subject to the constraint that the stress < allowable stress. Is the allowable stress Yield or Ultimate?
Any optimization problem needs to clearly define what can change to reduce the weight and satisfy the constraint. ANSYS includes Design Explorer software that can optimize design problems using some automation to search for the optimum set points for the parameters.
1) Is the location of the remote force always in the same place, or does it move around?
2) Is the direction of the remote force always the same or does it vary?
3) What design parameters can be modified to change the result?
a) Wall thickness
b) Diameter
c) Location along X axis
d) Location along Y axis, for example, could the three tubes be laid out in a triangle arrangement?
e) Can other materials be selected for the tubes?
4) What is the Fixed side of the tube connected to? How is it connected?
5) What is the Rigid side of the tube connected to? How is it connected?
6) Is there another constraint such as a maximum deflection at the remote point? For example, if the tube was aluminum instead of steel, the weight would be 1/3 that of steel tubes, but the deformation at the remote point would be 3 times larger.
Thank you for pointing out various considerations for the optimization of a structure. But the question still remains the same as it was before, will the forces experienced by the scoped rigid faces on each of the tube will be same or close to that of reality or not? Does the nature appoints the forces on the faces its scoped to in reality in the same way ANSYS is doing?
ANSYS creates a mathematical model, based on your inputs, and the solver finds equilibrium to a high degree of precision. That means all the forces computed precisely balance the applied force.
Accuracy has to do with how closely the mathematical model represents the physical reality. You are idealizing the physical reality by replacing a physical object with an idealized representation. You are taking away a physical object that distributes the force among three tube and replacing it with a perfectly rigid mathematical object. Hopefully, that is a good representation, but that is up to you. An alternative is to represent that object in the model and allow its flexibility to be included in the calculations.
@peteroznewman, hello again on this thread.
So even if I put a fixed support on a face of a solid body, that face will not see any deformation i.e. no motion of the nodes, but still it will experience a stresses because of the nodes on that face have stress (coming from the integration points), am I correct?
Also, the main aim to get back to this thread was to ask this question. If you look back at the tubes analysis pictures I shared, you mentioned that the solver is responsible of finding the correct equilibrium happening in the structure and then distributing the forces according to that. I want to go in a little bit of detail here. So If the applied force is not passing through the centroid of the scoped faces, what I understood is that the applied force is shifted to the centroid of the scoped faces, and all of the faces will have now equal distribution of force (assuming the faces are of same area). Nevertheless, the shifting of force also triggers a moment generation. This moment then turns into additional forces acting on the faces (maybe depending on the direction in which the moment is caused). Is it correct? If it is, then how is this moment divided into the additional forces on the scoped faces? Are they equal? What equations should be satisfied within the solver to calculate the exact distribution of these additional forces on the scoped faces?
Secondly, if I apply an external moment instead of an external force, so still this moment is turned into a pair of forces acting on the scoped faces? Does the moment always do that?
a fixed support on a face of a solid body, that face will not see any deformation i.e. no motion of the nodes, but still it will experience a stresses because of the nodes on that face have stress (coming from the integration points)
a fixed support on a face of a solid body, that face will not see any deformation i.e. no motion of the nodes, but
stillitthe elements will experienceastresses becauseofthe nodes onthatthe opposite face havestressdeformations (coming fromcreating stress at the integration points).So If the applied force is not passing through the centroid of the scoped faces, what I understood is that the applied force is shifted to the centroid of the scoped faces, and all of the faces will have now equal distribution of force (assuming the faces are of same area).
No, the faces will not have an equal distribution of force, even if they have the same area. A special case when equal distribution of force could happen is when the rigid remote force origin passes through the centroid of the three areas and the direction is parallel to the tube axis. This setup is what you might call a zero moment configuration.
When the force moves away from the centroid of the three faces (or tilts), the forces reduce on one side and increase in the opposite side. Yes, you could replace the offset force with a force and moment at the centroid. The solver just does its thing to solve for the static equilibrium.
A moment applied to a face of a solid body is always resolved to nodal forces over the area of the face of that solid body. Only Beam and Shell Elements can have a moment input to a vertex or an edge that is directly applied to nodes as a moment.
@Rameez_ul_Haq
@peteroznewman, well thank you :)